Is there a way to single point thread and then go back and thread it again but cut deeper threads on the next run?
I saw CNCKeith’s video where he did some threading, moved the spindle around and reran the program and it ran perfectly without damaging the existing threads. My question would involve editing the gcode or, preferably, editing the file using Intercon. So, as that is not the same thing, I’m not really sure if this will work? The encoder knows the position of the spindle but if you run a new (or edited) program, I would think it would disregard the known position?
Recutting single point threads
Moderator: cnckeith
-
- Posts: 595
- Joined: Tue Sep 12, 2017 10:03 pm
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: No
- Oak CNC controller: No
- CNC Control System Serial Number: 1030090099
- DC3IOB: Yes
- CNC12: Yes
- CNC11: Yes
- CPU10 or CPU7: No
- Location: Outside Winston-Salem, NC
- Contact:
Re: Recutting single point threads
Yes you can, as long as you do NOT move the part in the chuck/collet, and you don't change the Z position in the file. This has been my experience with all machine tools.I have not tested this in a Centroid machine, but If you don't change the start of the thread it should always start at the same point. You can actually see this in the G code file before you attempt it.ScotY wrote: ↑Tue Feb 06, 2018 3:30 am Is there a way to single point thread and then go back and thread it again but cut deeper threads on the next run?
I saw CNCKeith’s video where he did some threading, moved the spindle around and reran the program and it ran perfectly without damaging the existing threads. My question would involve editing the gcode or, preferably, editing the file using Intercon. So, as that is not the same thing, I’m not really sure if this will work? The encoder knows the position of the spindle but if you run a new (or edited) program, I would think it would disregard the known position?
Write the Intercon program, look at the start of the thread in X and Z, then modify the file for the start and finish diameter. Post and look at the start in X/Z.
Pretty straight forward to confirm.
Obviously you cannot change the pitch.
Clay
Clay
near Winston-Salem, NC
unofficial ACORN fb group https://www.facebook.com/groups/897054597120437/
near Winston-Salem, NC
unofficial ACORN fb group https://www.facebook.com/groups/897054597120437/
-
- Posts: 52
- Joined: Wed Nov 23, 2011 11:04 am
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: No
- Oak CNC controller: No
- CNC Control System Serial Number: K2019,K1110
- DC3IOB: No
- CNC11: No
- CPU10 or CPU7: Yes
- Location: Finger Lakes, NY
Re: Recutting single point threads
we have a T400 and just adjust the wear offset to cut deeper no modifying any files intercon or posted gcode, works excellent for fitting gun barrels to receivers right on the lathe
Ron
Ron
-
- Posts: 237
- Joined: Mon Nov 20, 2017 10:13 am
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: No
- Oak CNC controller: No
- CNC Control System Serial Number: none
- DC3IOB: No
- CNC11: Yes
- CPU10 or CPU7: Yes
- Location: Frenchville, PA
Re: Recutting single point threads
For threading cutting if the mating part does not fit all you have to do for an OD thread is use the Tool Wear offset and offset down (negative direction) to adjust to get the part or thread gage to go. For an ID thread offset up (positive direction). If you change the program starting Z the threads will be ruined if you try to re-cut the same part. You can change the ending Z in the program to cut the thread longer or shorter and that will not effect the thread. The control keeps tract of the spindle encoder and the Z positions for starting position. Re-posting the program will not effect the thread as long as the Z start position and/or in Intercon the Thread Angle is not changed . If the control is homed to reference marks and the machine is powered down you will not be able to re-cut the threads on that same part. The lathe in the video homes to switches that are a plunger type that are very repeatable.
Dana
When requesting support, please ALWAYS post a current report.
Need support? READ THIS POST first. http://centroidcncforum.com/viewtopic.php?f=60&t=1043
All Acorn Documentation is located here: viewtopic.php?f=60&t=3397
Answers to common questions: viewforum.php?f=63
and here viewforum.php?f=61
When requesting support, please ALWAYS post a current report.
Need support? READ THIS POST first. http://centroidcncforum.com/viewtopic.php?f=60&t=1043
All Acorn Documentation is located here: viewtopic.php?f=60&t=3397
Answers to common questions: viewforum.php?f=63
and here viewforum.php?f=61
-
- Posts: 654
- Joined: Sat Sep 23, 2017 7:57 pm
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: No
- Oak CNC controller: No
- CNC Control System Serial Number: none
- DC3IOB: No
- CNC11: No
- CPU10 or CPU7: No
- Location: Honolulu, HI
Re: Recutting single point threads
Thank you all for the information...very good to know this can be done! Modifying the wear offset seems to me to be the easiest way to go about it.